A single stiffened panel case

General Questions
1

Hi,
I made a simple stiffened panel model (see below). The loads and boundaries are simple, however, I can not get it converged, it always stops due to the increment required is too small (1e-9 or even less). Why so? The corresponding Abaqus run was finished smoothly.

I can not upload file and just pasted key inputs here. It will great if someone can shed light here.

A stiffened panel:
T-shaped stiffener, h: 180 mm, bf: 29.9 mm, tf: 20.6 mm. t_web: 8 mm, t_plate: 10 mm. b_plate: 780 mm. mesh size is about 50 mm.

Regards
H.Liu

\*\*
\*\* Heading +++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Heading
Hash: Y3MoWWWT, Date: 03/04/2026, Unit system: MM_TON_S_C
\*\*
\*\* Nodes +++++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Node
1, 0.00000000E+000, -3.90000000E+002, 0.00000000E+000
2, 5.00000000E+001, -3.90000000E+002, 0.00000000E+000
…
1430, 3.20000000E+003, 1.49500000E+001, -1.59400000E+002
\*\*
\*\* Elements ++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Element, Type=S4R, Elset=Shell_part-1
1, 1, 2, 3, 4
2, 4, 3, 5, 6
…
1343, 1427, 1429, 1300, 1297
1344, 1297, 1300, 1430, 1428
\*\*
\*\* Node sets +++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Nset, Nset=ALL_NODES
…
\*Nset, Nset=N_ENDS
…
\*Nset, Nset=N_EDGES
…
\*Nset, Nset=Internal-1_Internal_Selection-1_Pressure-1
…
\*Elset, Elset=Internal-1_Internal_Selection-1_Pressure-1_S2
…
\*\*
\*\* Surfaces ++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Surface, Name=Internal_Selection-1_Pressure-1, Type=Element
Internal-1_Internal_Selection-1_Pressure-1_S2, S2
\*\*
\*\* Physical constants ++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Coordinate systems ++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Materials +++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Material, Name=STEEL_S235
\*Density
7.85E-09
\*Elastic
210000, 0.3
\*Plastic
235, 0
360, 0.15
450, 0.5
\*DAMPING, ALPHA=5.0, BETA=1.0e-5
\*\*
\*\* Sections ++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Shell section, Elset=E_PLATE, Material=STEEL_S235, Offset=0
10
\*Shell section, Elset=E_WEB, Material=STEEL_S235, Offset=0
8
\*Shell section, Elset=E_FLANGE, Material=STEEL_S235, Offset=0
20.6
\*\*
\*\* Pre-tension sections ++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Constraints +++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Surface interactions ++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Contact pairs +++++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Amplitudes ++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Amplitude, Name=BLAST_AMP, Time=Total time
0, 0, 0.025, 1, 0.05, 0, 0.15, 0
\*\*
\*\* Initial conditions ++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Steps +++++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Step-2 ++++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Step, Nlgeom, Inc=10000
\*Dynamic
0.01, 1, 1E-08, 1E+30
\*\*
\*\* Controls ++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Output frequency ++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Boundary conditions +++++++++++++++++++++++++++++++++++++
\*\*
\*Boundary, op=New
\*\* Name: Displacement_rotation-1
\*Boundary
N_ENDS, 1, 1, 0
N_ENDS, 2, 2, 0
N_ENDS, 3, 3, 0
N_ENDS, 4, 4, 0
N_ENDS, 5, 5, 0
N_ENDS, 6, 6, 0
\*\* Name: Displacement_rotation-2
\*Boundary
N_EDGES, 2, 2, 0
\*\* Name: Displacement_rotation-3
\*Boundary
N_EDGES, 4, 4, 0
\*\* Name: Displacement_rotation-4
\*Boundary
N_EDGES, 6, 6, 0
\*\*
\*\* Loads +++++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Cload, op=New
\*Dload, op=New
\*\* Name: Pressure-1
\*Dload, Amplitude=BLAST_AMP
Internal-1_Internal_Selection-1_Pressure-1_S2, P2, -0.45
\*\*
\*\* Defined fields ++++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* History outputs +++++++++++++++++++++++++++++++++++++++++
\*\*
\*\*
\*\* Field outputs +++++++++++++++++++++++++++++++++++++++++++
\*\*
\*Node file
RF, U, V
\*El file
S, E, ENER, NOE
\*\*
\*\* End step ++++++++++++++++++++++++++++++++++++++++++++++++
\*\*
\*End step
2

Because of IP or forum restrictions for new users ? The latter has changed now - you should be able to upload files. But you could use a hosting service too.

We need a full input deck or better .pmx file to diagnose the issue. Non-convergence can have many causes.

3

Ok, thanks for the prompt reply. Here it is
.pmx file

.inp file:

4

Here are some remarks:

  1. You have *DAMPING, ALPHA=…, BETA=… at the material level. In CalculiX, only structural damping is defined at this level and Rayleigh damping is applied globally (can be defined when editing a dynamic step in PrePoMax).
  2. Dynamic implicit step in CalculiX is prone to convergence issues. Explicit isn’t, but has other issues (is slow and has some significant limitations - e.g. no rigid body constraints for 2D elements).
  3. Constraining rotational DOFs for shells in CalculiX is risky due to how it handles the drilling DOF. It’s especially problematic for curved shell edges where it may cause convergence issues and artificial stress concentrations.
  4. You can use shell section offsets to avoid material overlap:

image
image637×558 22.2 KB

image
image606×576 21.6 KB

  1. Considering the known issues with shell elements in CalculiX, it might be better to use solid elements instead (you can use the Thicken Shell Mesh tool in PrePoMax).
  2. It’s better to add nonlinearities gradually. So e.g. remove Nlgeom/plasticity and see if it works. You may also need to extrapolate plasticity (otherwise, it reaches plateau outside of the specified range).
  3. You could try a linear model first using the Modal Dynamics step.
1 Like